**CYCLE93 Introduction**

With the grooving (CYCLE93) cycle, you can make symmetrical and asymmetrical grooves for longitudinal and face machining on straight contour elements. You can machine both

external and internal grooves.

**CYCLE93 Format**

CYCLE93 (SPD, SPL, WIDG, DIAG, STA1, ANG1, ANG2, RCO1, RCO2, RCI1, RCI2, FAL1, FAL2, IDEP, DTB, VARI, _VRT, _DN) |

**Parameters**

SPD = Starting point in the facing axis (enter without sign) |

SPL = Starting point in the longitudinal axis |

WIDG = Groove width (enter without sign) |

DIAG = Groove depth (enter without sign) |

STA1 = Angle between contour and longitudinal axis; Range of values: 0 ≤ STA1 ≤ 180 degrees |

ANG1 = Flank angle 1: on the groove side determined by the starting point (enter without sign); Range of values: 0 ≤ ANG1 < 89.999 degrees |

ANG2 = Flank angle 2: on the other side (enter without sign) ; Range of values: 0 ≤ ANG2 < 89.999 |

RCO1 = Radius/chamfer 1, externally: on the side determined by the starting point |

RCO2 = Radius/chamfer 2, externally |

RCI1 = Radius/chamfer 1, internally: on the starting point side |

RCI2 = Radius/chamfer 2, internally |

FAL1 = Finishing allowance at the recess base |

FAL2 = Finishing allowance at the flanks |

IDEP = Infeed depth (enter without sign) |

DTB = Dwell time at recess base |

VARI = Machining type; Range of values: 1…8 and 11…18 |

_VRT = Variable retraction distance from contour, incremental (enter without sign) |

_DN = D number for 2nd edge of tool |

**CYCLE93 Examples**

**CYCLE93 CNC Program Example – 1 – Plunge Cutting**

This program is used to produce a groove externally at an oblique line in the longitudinal direction. The starting point is on the right-hand side at X35 Z60. The cycle uses tool offsets D1 and D2 of tool T1. The cutting tool must be defined accordingly.

Siemens CNC Turning CYCLE93 Program Example**DEF REAL SPD=35, SPL=60, WIDG=30, DIAG=25, STA1=5, ANG1=10, ANG2=20, RCO1=0, RCI1=-2, RCI2=-2, RCO2=0, FAL1=1, FAL2=1, IDEP=10, DTB=1 ; **Definition of parameters with value assignments

**DEF INT VARI=5 ;** Definition of parameters with value assignments

**N10 G0 G18 G90 Z65 X50 T1 D1 S400 M3 ;** Starting point before the beginning of the cycle

**N20 G95 F0.2 ;** Specification of technology values

**N30 CYCLE93 (SPD, SPL, WIDG, DIAG, STA1, ANG1, ANG2, RCO1, RCO2, RCI1, RCI2, FAL1, FAL2, IDEP, DTB, VARI) ;** Cycle call

**N40 G0 G90 X50 Z65 ;** Next position

**N50 M02 ;** Program end